Loft and Fusing Parts

[andrigtmiller]

OS: "Fedora release 25 (Twenty Five)"
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.16.Unknown
Build type: Unknown
Python version: 2.7.11
Qt version: 4.8.7
Coin version: 3.1.3
OCC version: 6.8.0.oce-0.17

I am trying to create a model with a radius rectangle that tapers down to a smaller radius rectangle between two other structures. Here is a picture of what I want it to look like:

[img]

Loft.png (43.74 KiB) Viewed 2022 times

[/img]

Now, this all looks correct, but the model has three parts, and I need to fuse them together, but as I discovered, you cannot fuse a loft, consider a shell, to a solid, so no amount of playing around with different techniques will make this come out as one part, unless I do something to somehow make the loft a solid.

In digging around on the forums I found someone trying to make their loft be 2mm thick, which is exactly what I want, in that I need the sides to be 2mm thick to match the two parts on either side, which are also 2mm thick.

In following the instructions, I made created another two sketches that were 2mm smaller than the original two sketches for the first loft. Then I made a secon loft. I made the first, and bigger loft (or outer) solid, and tried to do a cut between the two lofts, which is what the other forum post said to do. That doesn't work no matter which loft I make solid, or even both of them solid, a cut operation fails.

An intersection, with the outer loft being solid and the smaller inner loft not being solid sort of worked, but it doesn't have the 2mm thickness, and in fact it doesn't seem to have a thickness at all.

Unless, I can eventually make this into a solid, I certainly won't be able to fuse them into a single part.

I have also played around with making the different lofts ruled, closed, and the various combinations. I know there must be a way to do what I want, but I just cannot figure it out.

Any help is greatly appreciated.

[andrigtmiller]

Okay, sorry for the post, I just had another idea, with using a "cutout" between the inner and outer lofts, and that worked, and let me fuse the three parts together!

So, don't bother taking a look, I just got what I wanted.

[Willem]

Hi, instead of a fusion you can also make a compound in the Part workbench

Schermafdruk van 2017-02-22 23-43-57.png (261.04 KiB) Viewed 2011 times

[bejant]

I just had another idea, with using a "cutout" between the inner and outer lofts, and that worked, and let me fuse the three parts together!

That's still much more difficult than it needs to be. Here is the Dependency Graph for the model in your opening post:

20170222b.png (54.13 KiB) Viewed 2003 times

Instead I just edited and used your Sketches to create a solid of what would become the inside of the enclosure, selected the large end face and the two circular faces on the other side, then used the Part WB > Thickness tool to remove those faces and add 2 mm to the outside. It's a much simpler work flow:

20170222c.png (24.9 KiB) Viewed 2003 times

20170222a-016-bejant-HeaterCoreEnclosure.fcstd

(53.43 KiB) Downloaded 28 times

OS: Ubuntu 16.04.2 LTS
Word size of OS: 32-bit
Word size of FreeCAD: 32-bit
Version: 0.16.6707 (Git)
Build type: None
Branch: releases/FreeCAD-0-16
Hash: 5465bc47c95db45e0be85dc0e2872419efadce0f
Python version: 2.7.12
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17

[NormandC]

Blast! bejant was faster than me.

I'm posting anyway because I used a slightly different method, my thickness goes inward rather than outward.

you cannot fuse a loft, consider a shell, to a solid, so no amount of playing around with different techniques will make this come out as one part, unless I do something to somehow make the loft a solid.

This is accomplished by ticking the "Solid" checkbox at Loft creation. After the loft is done, you can still change the parameter in the Data tab.

Here's an alternate method that requires a lot less work than you solution: build everything as a solid, and at the end use Part Thickness to hollow the solid out. Just be aware that this tool is tricky and not very robust; sometimes it fails for no apparent reason. Here it works beautifully though.

Also look at the sketches I reworked to centre them on the origin without having to use so many dimensional constraints. The trick is to use a symmetric constraint between two diagonally opposed point and the sketch origin point.

Hi, instead of a fusion you can also make a compound in the Part workbench

A compound only groups separate solids together and does not really fuse them, which can be a problem for STL export, or if you need to apply further Booleans. It's not an appropriate use here.

[bejant]

Blast! bejant was faster than me.

Had I known you were working on the model too I could have saved myself some time. We abandoned it, but maybe we should go back to using our informal protocol again?
For anyone who is wondering (or who forgot) what that is:
viewtopic.php?f=8&t=5628&p=45565

[NormandC]

Good idea.

I admit to not looking who was online first. I shouldn't even reply to help requests on the forum right now, as I'm trying to reanimate this project. But when I see anything posted in the Help section I can't help it. My real interest here is to help others learn/use FreeCAD, not packaging the software and its libraries...

[andrigtmiller]

Thanks for the replies. I am learning a lot, and I appreciate the hep in making things simpler.

Andrig